Hi,
Our design involves two main boards; a 'core' module which contains the DM365, SDRAM, NAND and supply circuitry and a 'gateway' module onto which the 'core' module plugs via dual row 1.27mm pitch header pins and contains the TVP5146 Video Decoder, Micrel Ethernet Phy, battery backup etc. The goal with this was to confine the high speed routing and minimize the size (/expense) of a highly multilayer board of & reusable & modular 'core' module.
My question revolves around an uneasiness I have regarding taking the TVP5146 off the 'core' module and onto the lower 'gateway' module. This requires the tracks (YIN7 through YIN0, CIN7 through CIN0, and HD, VD, C_WE_FIELD & PCLK) being fed down through the 1.27mm pitch double header connector down to the gateway board before it is routed to the TVP5146 & the RCA connectors. Ie the tracks from the DM365 to the TVP5146 are longer than the tracks from the RCA connector to the TVP5146.
I have two options: TVP5146 close to the DM365 or TVP5146 close to the RCA connector. Logically, the highest frequency the raw analog video lines will carry for PAL, SECAM or NTSC will be around the 7MHz mark (correct?) whilst the BT.656 lines will be around the order of 13.5Mhz (Page 17 of SLES141D for the TVP5146) (correct?). I would prefer to keep the TVP5146 on the lower 'gateway' module. Would anyone care to entertain my concern and provide some input re the dangers of extending either the digitized or the raw analog lines or whether I should be concerned at all?
Many thanks,NickA
Nick,
This is always a tough question since it depends very much on your competing design requirements.
The ITU656 stream will be 27MHz in 8 bit mode or 13.5MHz in 16 bit mode. If you maintain good ground returns for these signals then you should be able to traverse long distances without too much trouble. The pixel frequency is 13.5MHz.
For the analog video you need to consider much more than the signal bandwidth. Since this is an analog signal it is necessary to make sure that it does not receive significant interference. If you decide to rout this signal over long distances then make sure that the coupling capacitor is clock to the TVP5146, that the signal trace is impedance matched to 75R, that you have a good and separate analog ground return and, if possible, run the signal on an inner layer, surrounded by your analog ground to effectively shield it from interference.
Personally I would tend to try and reduce the analog signal length since it is typically more difficult to protect this signal from undesired interference whereas the digital signals are fairly simple to control (good ground planes, no loops etc...)
You may also find the following articles useful...
http://www.speedingedge.com/RelatedArticles.htm
Hope this helps a little.
BR,
Steve
Please mark this post as answered via the Verify Answer button below if you think it answers your question. Thanks!
Hi Nick,
To guard against potential noise issues, our preference would be to not sacrifice the RCA>TVP5146 analog trace lengths. We have freqeuntly connected the TVP5146 digital outputs to other boards using both connectors and cables while operating at full 27MHZ 10-bit BT656 speed without problems. If you are using the 20-bit 13.5MHz 4:2:2 output format, you will have even more margin. We do recomend using series termination resistors on the digital traces placed close to the TVP5146. Try to avoid excessive trace length mismatch.
I agree with Larry and Steve,
The system can tolerate several inches of trace between the TVP and DM parts as long as you practice good PCB design. The traces should be referenced to a contiguous ground plane, and the connector should provide lots of ground pins for signal returns.
Hi Larry, Steve, Todd,
Thank you very much for all your quick replies. I appreciate the input.
Sincerely,NickA
Hello,
I am using DM365. I have following queries.
In the datasheet of TMS320DM365 only DDR2 impedance's are provided.
We need Impedance details of following pins also:
1. Cin & Yin (video in), HD,VD, PCLK,C_WE_FIELD, Tx/Rx serial port, DATA0/1/2/3 (SD card Lines), NAND Flash pins, Cout/Yout pins, VSYNC, HSYNC pins(Video out), etc.
2. We are using Leopard Imaging's DM365 board. The stack up they followed is different than TI's datasheet. So please suggest which is to be followed.
PCB stack up Leopard Board Vs. TI Datasheet:
Layer
Leopard board DM365
As per datasheet
Top Layer
Routing
Top Routing Mostly Horizontal
Inner layer 2
Gnd
Inner layer 3
Power
Inner layer 4
VCC2
Internal Routing
Inner layer 5
VCC
Bottom layer
Bottom routing mostly vertical
Please suggest which PCB stack up we should we follow?
3. Also let us know what other precautions need to be taken while designing PCB using DM365.
Please see this post...
http://e2e.ti.com/support/dsp/davinci_digital_media_processors/f/100/p/246577/865696.aspx#865696